Manufacturing DevBlog

Place total mass value from partslist in Title Block

By Augusto Goncalves

The mass values can be queried from Partslist and we can iterate through all rows and sum up all mass column values. We can create a custom property named "Mass" with PropID 99 and this property can be put into Title Block as TextBox object. We can also put some static text like "Total Weight" or "Total Mass" to the left of custom property.

The Advantage of using Custom property in Title Block is that it gets updated automatically when the property value is modified. The sample code demonstrates same.

If the drawing does not contain mass column in PartsList then you
can add one  by following the procedure shown below

1. Select PartsList
2. Right click and Select "Edit PartsList..."
3. Select Column Chooser Icon (2nd from left)
4. In the left Combo box select PartsList
5. At the list select "MASS" and click on "Add->" button

Sub UpdateMassInTitleBlock()

  ' The sample code calculates total

  ' weight from partslist and adds a

  ' custom property "mass" to drawing

  ' document, this custom property is

  ' then added to title block definition.

  ' Make sure that Mass column is

  ' added to partslist

 

  ' The custom property is added once

  ' to title block definition, whenever the

  ' value of custom property changes

  ' the value is automatically updated in

  ' Title block

 

  ' This sample should be tested on

  ' a drawing which has C/A2 sheet along

  ' With PartsList

  ' The co-ordinated of static text

  ' and property value are based on sheet size

 

  Dim oDoc As Document = _

    m_inventorApplication.ActiveDocument

 

  If (oDoc.DocumentType = DocumentTypeEnum. _

      kDrawingDocumentObject) Then

    Dim oDrgDoc As DrawingDocument

    oDrgDoc = oDoc

    'sum up the mass from partslist

    Dim oPartsList As PartsList

    oPartsList = oDrgDoc.ActiveSheet. _

      PartsLists.Item(1)

    ' Assuming that last column is mass

    Dim dTotalWt As Double

    For i = 1 To oPartsList.PartsListRows.Count

      Dim nColInd As Long

      nColInd = oPartsList.PartsListColumns.Count

      ' get weight from column , it also contains units

      Dim sVal As String

      sVal = oPartsList.PartsListRows. _

        Item(i).Item(nColInd).ToString() ' CHNAGE 1

      Dim pos As Integer

      pos = InStrRev(sVal, " ")

      ' Get the units of mass value

      Dim sUnits As String

      sUnits = Mid(sVal, pos + 1)

      sVal = LSet(sVal, pos - 1) 'chnage 2

      If (sUnits = "lbmass") Then

        dTotalWt = dTotalWt + CDbl(sVal) _

          * (1.0# / 2.2) 'convert to Kg

      Else

        dTotalWt = dTotalWt + CDbl(sVal)

      End If

    Next

 

    ' Add the custom property mass if not present

    ' Get User Defined propertySet

    Dim oPropSet As PropertySet

    oPropSet = oDoc.PropertySets(

      "User Defined Properties")

 

    Dim oProp As Inventor.Property

    oProp = oPropSet.ItemByPropId(99)

 

    'change 2

    Try

      Call oPropSet.Add(dTotalWt, "Mass", 99)

    Catch ex As Exception

      oProp.Value = dTotalWt

    End Try

 

    ' Check whether 'Total Weight' label is present

    Dim oTitleDef As TitleBlockDefinition

    oTitleDef = oDrgDoc.ActiveSheet. _

      TitleBlock.Definition

 

    Dim oTextB As TextBox

    For Each oTextB In oTitleDef.Sketch.TextBoxes

      If oTextB.Text = "Total Weight" Then

        oDoc.Save()

        Exit Sub

      End If

    Next

 

    Dim oTG As TransientGeometry

    oTG = m_inventorApplication.TransientGeometry

 

    'Start edit of Title Block

    Dim oSketch As DrawingSketch = Nothing

    Call oTitleDef.Edit(oSketch)

 

    ' Add static text

    Dim sText As String

    sText = "<StyleOverride FontSize='.35'>" + _

      "Total Weight</StyleOverride>"

    Dim oTextBox As TextBox

    oTextBox = oSketch.TextBoxes.AddFitted(

      oTG.CreatePoint2d(43, 5), sText)

    oTextBox.VerticalJustification = _

      VerticalTextAlignmentEnum.kAlignTextMiddle

    oTextBox.HorizontalJustification = _

      HorizontalTextAlignmentEnum.kAlignTextLeft

 

    ' Add some property Value

    ' In the statement below Property

    ' Document= 'drawing' means that

    ' custom property is part of this

    ' drawing document.

    ' FormatID is GUID of User

    ' Defined(properties)

    ' Finally value 99 in PropertyID

    ' is value we assigned to Mass property

 

    ' The property value updates

    ' automatically in the title block when

    ' the value of property is modified.

    ' GUID of user defined properties

    '{D5CDD505-2E9C-101B-9397-08002B2CF9AE}

    sText = "<StyleOverride FontSize='0.35'>" + _

      "<Property Document='drawing' " + _

      "FormatID=" + _

      "'{D5CDD505-2E9C-101B-9397-08002B2CF9AE}' " + _

      "PropertyID='99' /></StyleOverride>"

    oTextBox = oSketch.TextBoxes.AddFitted( _

      oTG.CreatePoint2d(46, 5), sText)

    oTextBox.VerticalJustification = _

      VerticalTextAlignmentEnum.kAlignTextMiddle

    oTextBox.HorizontalJustification = _

      HorizontalTextAlignmentEnum.kAlignTextLeft

 

    ' End editing

    Call oTitleDef.ExitEdit(True)

  End If

End Sub

Create a Flush Constraint between Two Faces Using C++

By Barbara Han

Issue
How to create a flush constraint between two faces using C++?

Solution
The following code creates a flush constraint for the first faces of the first two occurrences.
Please make sure that these faces are planar, not e.g. the side of a cylinder.

static HRESULT GetInventorInformation()
{
    HRESULT Result = NOERROR;

    TCHAR Str[_MAX_PATH];
   
    CLSID InvAppClsid;
    Result = CLSIDFromProgID (L"Inventor.Application", &InvAppClsid);
    if (FAILED(Result)) return Result;

    // 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'))
    {
        Result = CoCreateInstance (InvAppClsid, NULL, CLSCTX_LOCAL_SERVER, __uuidof(IUnknown), (void **) &pInvAppUnk);
        if (FAILED (Result))
            _tprintf_s (_T("*** Failed to create a new Inventor application ***\n"));
    }
    else
    {
        Result = ::GetActiveObject (InvAppClsid, NULL, &pInvAppUnk);
        if (FAILED (Result))
            _tprintf_s (_T("*** Could not get hold of an active Inventor application ***\n"));
    }
    if (FAILED(Result)) return Result;

    CComPtr<Application> pInvApp;
    Result = pInvAppUnk->QueryInterface (__uuidof(Application), (void **) &pInvApp);
    if (FAILED(Result)) return Result;

    CComPtr<Document> pDoc;
    Result = pInvApp->get_ActiveDocument(&pDoc);
    if (FAILED(Result)) return Result;

    CComQIPtr<AssemblyDocument> pAsmDoc(pDoc);
    CComPtr<AssemblyComponentDefinition> pCD;
    Result = pAsmDoc->get_ComponentDefinition(&pCD);
    if (FAILED(Result)) return Result;

    CComPtr<AssemblyConstraints> pACs(pCD->Constraints);

    CComPtr<Face> pFace1(pCD->Occurrences->Item[1]->SurfaceBodies->Item[1]->Faces->Item[1]);
    CComPtr<Face> pFace2(pCD->Occurrences->Item[2]->SurfaceBodies->Item[1]->Faces->Item[1]);

    CComVariant varEmpty, varReal(0.0);

    // add the constraint
    CComPtr<FlushConstraint> pFC;   
    Result = pACs->AddFlushConstraint(pFace1, pFace2, varReal, varEmpty, varEmpty,&pFC);
    if (FAILED(Result)) return Result;
    return true;
}

Use OnTranslateDocument event to get notification when user exports to IGES

By Wayne Brill

If you need to get a notification when the user exports to other formats such as IGES, STEP or SAT use the ApplicationEvents.OnTranslateDocument event. This event is fired when a document is translated to a different format. The code snippet below is a C# example.

This SDK project shows how to use events in VB.NET:

C:\Users\Public\Documents\Autodesk\Inventor 2013\SDK\DeveloperTools\Tools\EventWatcher

C# code snippet:

  private void InitEvent()

        {

            oAppEvents = _invApp.ApplicationEvents;

            oAppEvents.OnTranslateDocument +=

            new

ApplicationEventsSink_OnTranslateDocumentEventHandler

                     (oAppEvent_OnTranslateDocument);

 

        }

 

        void oAppEvent_OnTranslateDocument

            (bool TranslatingIn,

             Inventor._Document DocumentObject,

             string FullFileName,

             EventTimingEnum BeforeOrAfter,

             NameValueMap Context,

             out HandlingCodeEnum HandlingCode)

        {

            string extension =

     System.IO.Path.GetExtension(FullFileName);

            if (extension == ".igs")

            {

                System.Windows.Forms.

     MessageBox.Show("saving to a .igs file");

            }

            else if (extension == ".jpg")

            {

                System.Windows.Forms.

   MessageBox.Show("saving to a .jpg file");

            }

 

            HandlingCode =

          HandlingCodeEnum.kEventNotHandled;

        }

Document.Thumbnail property always fails using Inventor API from out of process

By Wayne Brill

The Document.Thumbnail property will always return nothing when called from an out of process application. There is a known Microsoft limitation on marshalling bitmaps across COM APIs between two processes. If your VB application runs out-of-process of Inventor process, then you hit the Microsoft limitation. Also if you are debugging an in-process client application (e.g. Inventor AddIn), then the VB environment actually creates an out-of-process exe as part of the debugging process, this would also prevent you from marshalling bitmaps across the API.

Usually you can use one of the following several ways to avoid that problem:
1. Use Apprentice because it's running in its own process. (VBA 32 bit runs in the same process with Inventor but not 64bit). 
This post shows how to use Apprentice to get the thumbnail.

2. Create an in-process Addin application (DLL addin) - Note for this way, running the Addin application (not debug) is ok, but if you debug the application from VB or .net IDE, you still need to comment out the codes relevant to the thumbnail picture interface so your application can be loaded in Inventor successfully, at last comment in those thumbnail picture related codes before releasing your application.

This Mod The Machine post has more information about this issue.

How to Determine Which Drawing Dimensions Belong to a Particular View

By Barbara Han

Issue

I want to be able to determine or sort out which drawing dimensions belongs to a view in a drawing. Is there an example that shows how this can be done?

Solution

A DrawingDimension object is not directly related to a particular view, they are just annotations on a Sheet. So there is not a direct way to determine which View a DrawingDimension belongs to.

However you can reach this information through the "Intent" property of the GeneralDimension, which is dependent of the View.

Here is a VBA example that you can run on a drawing document. It will iterate through the DrawingDimensions of the sheet and find out if the dimension belongs to a given View, based on the view's name:

VBA:

Public Function GetDrawingDimForView(oSheet As Sheet, ViewName As String) As ObjectCollection
    Dim oDrawDimsForView As ObjectCollection
    Set oDrawDimsForView = ThisApplication.TransientObjects.CreateObjectCollection
   
    Dim oDrawDims As DrawingDimensions
    Set oDrawDims = oSheet.DrawingDimensions
   
    Dim oDrawDimIterator As DrawingDimension
    For Each oDrawDimIterator In oDrawDims
        Select Case oDrawDimIterator.Type
        Case kLinearGeneralDimensionObject
            Dim oLinearDim As LinearGeneralDimension
            Set oLinearDim = oDrawDimIterator
            If oLinearDim.IntentOne.Geometry.Parent.Name = ViewName Then
                oDrawDimsForView.Add oDrawDimIterator
            End If
        Case kRadiusGeneralDimensionObject
            Dim oRadiusDim As RadiusGeneralDimension
            Set oRadiusDim = oDrawDimIterator
            If oRadiusDim.Intent.Geometry.Parent.Name = ViewName Then
                oDrawDimsForView.Add oDrawDimIterator
            End If
        Case kDiameterGeneralDimensionObject
            Dim oDiameterDim As DiameterGeneralDimension
            Set oDiameterDim = oDrawDimIterator
            If oDiameterDim.Intent.Geometry.Parent.Name = ViewName Then
                oDrawDimsForView.Add oDrawDimIterator
            End If
        Case kAngularGeneralDimensionObject
            Dim oAngularDim As AngularGeneralDimension
            Set oAngularDim = oDrawDimIterator
            If oAngularDim.IntentOne.Geometry.Parent.Name = ViewName Then
                oDrawDimsForView.Add oDrawDimIterator
            End If
        Case Else
        'Case is not handled...
        End Select
    Next
    Set GetDrawingDimForView = oDrawDimsForView
End Function

'Test function GetDrawingDimForView
Public Sub TestGetDrawingDimensions()
    Dim oDoc As DrawingDocument
    Set oDoc = ThisApplication.ActiveDocument
    Dim oDrawingDimCollec1 As ObjectCollection
    Set oDrawingDimCollec1 = GetDrawingDimForView(oDoc.ActiveSheet, "VIEW1")
    Dim oDrawingDimCollec2 As ObjectCollection
    Set oDrawingDimCollec2 = GetDrawingDimForView(oDoc.ActiveSheet, "VIEW2")
End Sub

VB.NET:

Public Function GetDrawingDimForView(ByVal oSheet As Sheet, ByVal ViewName As String) As ObjectCollection

  Dim oDrawDimsForView As ObjectCollection

  oDrawDimsForView = _InvApplication.ActiveDocument.TransientObjects.CreateObjectCollection

  Dim oDrawDims As DrawingDimensions

  oDrawDims = oSheet.DrawingDimensions

  Dim oDrawDimIterator As DrawingDimension

  For Each oDrawDimIterator In oDrawDims

    Select Case oDrawDimIterator.Type

      Case kLinearGeneralDimensionObject

        Dim oLinearDim As LinearGeneralDimension

        oLinearDim = oDrawDimIterator

        If oLinearDim.IntentOne.Geometry.Parent.Name = ViewName Then

          oDrawDimsForView.Add(oDrawDimIterator)

        End If

 

      Case kRadiusGeneralDimensionObject

        Dim oRadiusDim As RadiusGeneralDimension

        oRadiusDim = oDrawDimIterator

        If oRadiusDim.Intent.Geometry.Parent.Name = ViewName Then

          oDrawDimsForView.Add(oDrawDimIterator)

        End If

 

      Case kDiameterGeneralDimensionObject

        Dim oDiameterDim As DiameterGeneralDimension

        oDiameterDim = oDrawDimIterator

        If oDiameterDim.Intent.Geometry.Parent.Name = ViewName Then

          oDrawDimsForView.Add(oDrawDimIterator)

        End If

 

      Case kAngularGeneralDimensionObject

        Dim oAngularDim As AngularGeneralDimension

 

        oAngularDim = oDrawDimIterator

 

        If oAngularDim.IntentOne.Geometry.Parent.Name = ViewName Then

 

          oDrawDimsForView.Add(oDrawDimIterator)

 

        End If

 

      Case Else

 

        'Case is not handled...

 

    End Select

 

  Next

 

  GetDrawingDimForView = oDrawDimsForView

 

End Function

 

'Test function GetDrawingDimForViewPublic

Sub TestGetDrawingDimensions()

  Dim oDoc As DrawingDocument

  oDoc = _InvApplication.ActiveDocument.ActiveDocument

  Dim oDrawingDimCollec1 As ObjectCollection

  oDrawingDimCollec1 = GetDrawingDimForView(oDoc.ActiveSheet, "VIEW1")

  Dim oDrawingDimCollec2 As ObjectCollection

  oDrawingDimCollec2 = GetDrawingDimForView(oDoc.ActiveSheet, "VIEW2")

End Sub

In the case where you have to deal with dimensions that are not GeneralDimensions, the function above is no longer valid and you have no means to sort out these dimensions through that way. However you can still check the "Annotations Visibility->Drawing Dimensions" setting by right-clicking on a view to activate the dimensions on this particular view, and uncheck the same setting on other views. Then if you run this code:

Dim oDoc As DrawingDocumentSet
oDoc = ThisApplication.ActiveDocument
Dim oDrawDims As DrawingDimensionsSet
oDrawDims = oDoc.ActiveSheet.DrawingDimensions
You will get the complete set of DrawingDimensions that are in the specified view.

Creating constraint in Assembly

By Augusto Goncalves

The first sample demonstrates the creation of an assembly mate constraint. Before running the sample, you need to open an assembly that contains at least two parts. Select planar faces on the two parts that will be used for the constraint and run the sample code (Set the priority of the Select command and use the Shift-Select to select multiple faces).

Then the second sample demonstrates creating a mate constraint between two occurrences using the work planes within those occurrences. To use the sample,  have an assembly open that contains at least two occurrences (part or subassembly), and run the program.

private void MateConstraint()

{

  //Set a reference to the assembly component definintion.

  AssemblyDocument oAssDoc =

    m_inventorApp.ActiveDocument as AssemblyDocument;

  AssemblyComponentDefinition oAsmCompDef =

    oAssDoc.ComponentDefinition;

 

  // Set a reference to the select set.

  SelectSet oSelectSet = m_inventorApp.ActiveDocument.SelectSet;

 

  //Validate the correct data is in the select set.

  if (oSelectSet.Count != 2)

  {

    System.Windows.Forms.MessageBox.Show(

      "You must select the two entities valid for mate.");

  }

 

  // Get the two entities from the select set.

  object oBrepEnt1 = oSelectSet[1];

  object oBrepEnt2 = oSelectSet[2];

 

  //Create the insert constraint between the parts.

  MateConstraint oMate = oAsmCompDef.Constraints.

    AddMateConstraint(oBrepEnt1, oBrepEnt2, 0,

    InferredTypeEnum.kNoInference,

    InferredTypeEnum.kNoInference, null, null);

}

 

private void MateConstraintOfWorkPlanes()

{

  AssemblyDocument oAssDoc =

    m_inventorApp.ActiveDocument as AssemblyDocument;

  AssemblyComponentDefinition oAsmCompDef =

    oAssDoc.ComponentDefinition;

 

  //Get references to the two occurrences to constrain.

  //This arbitrarily gets the first and second occurrence.

  ComponentOccurrence oOcc1 = oAsmCompDef.Occurrences[1];

  ComponentOccurrence oOcc2 = oAsmCompDef.Occurrences[2];

 

  PartComponentDefinition oPartDef1 =

    oOcc1.Definition as PartComponentDefinition;

  PartComponentDefinition oPartDef2 =

    oOcc2.Definition as PartComponentDefinition;

 

  // Get the XY plane from each occurrence. This goes to the

  //component definition of the part to get this information.

  //This is the same as accessing the part document directly.

  //The work plane obtained is in the context of the part,

  // not the assembly.

  WorkPlane oPartPlane1 = oPartDef1.WorkPlanes[3];

  WorkPlane oPartPlane2 = oPartDef2.WorkPlanes[3];

 

  // Because we need the work plane in the context of the assembly

  //we need to create proxies for the work planes. The proxies

  // represent the work planes in the context of the assembly.

  object obj1;

  oOcc1.CreateGeometryProxy(oPartPlane1, out obj1);

  WorkPlaneProxy oAsmPlane1 = (WorkPlaneProxy)obj1;

  object obj2;

  oOcc2.CreateGeometryProxy(oPartPlane2, out obj2);

  WorkPlaneProxy oAsmPlane2 = (WorkPlaneProxy)obj2;

 

  //Create the constraint using the work plane proxies.

  oAsmCompDef.Constraints.AddMateConstraint(oAsmPlane1,

    oAsmPlane2, 0, InferredTypeEnum.kNoInference,

    InferredTypeEnum.kNoInference, null, null);

}

How to use private storage and stream in C++

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 want to use Inventor API, please refer to the other article. 

MSDN: "The IStorage interface supports the creation and management of structured storage objects. Structured storage allows hierarchical storage of information within a single file, and is often referred to as "a file system within a file". Elements of a structured storage object are storages and streams. Storages are analogous to directories, and streams are analogous to files. Within a structured storage there will be a primary storage object that may contain substorages, possibly nested, and streams. Storages provide the structure of the object, and streams contain the data, which is manipulated through the IStream interface."

The Inventor API allows the use of Private Storages and Streams inside Inventor documents, but it encapsulates the COM Interfaces IStorage and IStream in a way that make it easier to manipulate.

For further details about the COM interfaces, please refer to the online Microsoft documentation:

IStorage: http://msdn2.microsoft.com/en-us/library/aa380015.aspx
IStream: http://msdn2.microsoft.com/en-us/library/aa380034.aspx

Important Notes:

- When Inventor opens a file, it reads in the embedded streams and edit it in memory, and writes it back out on save. If you edit this storage using the Microsoft structured storage APIs directly on the file root storage opened off disk, your changes would be overwritten if the file was also opened in Inventor and saved after your changes.  Also changes made like this would not be realized in the in memory open document until the document is closed and reopened (if it was not saved and overwrote the changes). For this reason you should not use the Microsoft API directly on an open Inventor document, use the exposed Inventor API below instead.

- Also, manipulating the file storage is not a transacted operation, i.e. you cannot use the undo/redo mechanism after a change. For this reason, any modification to the file storage will not set it as 'Dirty', so simply saving and closing the file through Inventor will result in the lost of these changes. In order to keep the storage modifications across sessions, you will need to manually set the 'Dirty' flag to True prior to performing the save. This is illustrated in the sample below.  

The following C++ sample contains three methods that illustrate how to create a storage and a stream inside it, write and read from it and also delete the stream. It is from a standard alone EXE. It assumes Inventor has been launched.

// manipulate Private Stream

static HRESULT PrivateStream()

{

     HRESULT Result=NOERROR;

 

    Result = ::CoInitialize (NULL);

 

    // get active inventor application

   CLSID clsid;

   ::CLSIDFromProgID(L"Inventor.Application",

                        &clsid);

 

   CComPtr<IUnknown> pUnk;

   ::GetActiveObject(clsid,NULL,&pUnk);

 

   CComPtr<Application> pApp;

   Result = pUnk->QueryInterface(__uuidof(Application),

                                (void**)&pApp);

 

   // Get active Document

   CComPtr<Document> pDoc;

   Result = pApp->get_ActiveDocument(&pDoc);

 

    char outData[256];

    //COM Stream

    Result = CreatePrivateStorageAndStream(pDoc,

                                "MyPrvStorage1",

                                "MyStream1",

                                "Some private stored data");

 

   if(Result != S_OK)

  {

      //ERROR: unable to create Stream

      return Result;

  }

 

   Result = ReadPrivateStorageAndStream(pDoc,

                                    "MyPrvStorage1",

                                    "MyStream1",                                   

                                    outData);

 

   if(Result != S_OK)

  {

      //ERROR: unable to read Stream

      return Result;

  }

 

Result = DeletePrivateStream(pDoc,

                        "MyPrvStorage1",

                        "MyStream1");

 

 if(Result != S_OK)

{

  //ERROR: unable to delete Stream

  return Result;

}

 

 //Set document to Dirty prior to perform the Save

 //otherwise the stream won't be save through sessions

pDoc->Dirty = VARIANT_TRUE;

pDoc->Save();

 

 

wrapup:

::CoUninitialize();

}

//Create Private Storage And Stream

 static HRESULT CreatePrivateStorageAndStream(

                            CComPtr<Document> pDoc,

                             constchar* StorageName,

                             constchar* StreamName,

                             constchar* data)

{

     HRESULT hr;

 

    //Try to get Private Storage, if does not exist try to create

    CComPtr<IUnknown> pUnk;

    hr=pDoc->GetPrivateStorage(CComBSTR(StorageName),

                                 VARIANT_TRUE,&pUnk);

 

   if(hr != S_OK)

  {

       //ERROR: unable to create or open Storage

       return hr;

  }

 

  CComQIPtr<IStorage> pStg(pUnk);

 

  //Create stream within private storage

  CComPtr<IStream> pStream = NULL;

  hr=pStg->CreateStream(CComBSTR(StreamName),

                            STGM_DIRECT|STGM_CREATE|

                            STGM_READWRITE|STGM_SHARE_EXCLUSIVE,

                            0, 0, &pStream);

 

  if(hr != S_OK)

  {

       //ERROR: unable to create Stream

      return hr;

}

 

  ULONG lsize=0;

  lsize = strlen(data);

  hr=pStream->Write( &lsize,sizeof(int), NULL ) ;

  hr=pStream->Write( data, strlen(data), NULL ) ;

  // Save the data

  hr=pStream->Commit(STGC_DEFAULT|STGC_OVERWRITE);

 

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

   hr=pStg->Commit(STGC_DEFAULT|STGC_OVERWRITE);

 

   return hr;

}

 

// Read Private Storage And Stream

static HRESULT ReadPrivateStorageAndStream(CComPtr<Document> pDoc,

                                constchar* StorageName,

                                constchar* StreamName,

                                char* outData)

{

     HRESULT hr;

 

    //Try to get Private Storage, if does not exist fail

    CComPtr<IUnknown> pUnk;

    hr = pDoc->GetPrivateStorage(CComBSTR(StorageName),

                                    VARIANT_FALSE,&pUnk);

 

   if(hr != S_OK)

   {

      //ERROR: unable to open Storage

      return hr;

   }

 

   CComQIPtr<IStorage> pStg(pUnk);

 

   // Open stream within private storage

   CComPtr<IStream> pStream = NULL;

   hr = pStg->OpenStream(CComBSTR(StreamName),0,

                                    STGM_DIRECT|STGM_READ|

                                    STGM_SHARE_EXCLUSIVE, 0,

                                    &pStream);

 

   if(hr != S_OK)

  {

      //ERROR: unable to open Stream

      return hr;

   }

 

   ULONG lsize = 0;

   hr = pStream->Read( &lsize,sizeof(int), NULL);

   hr = pStream->Read( outData,lsize, NULL ) ;

 

   outData[lsize] = '\0';

 

   return hr;

}

 

// Delete Private Stream

static HRESULT DeletePrivateStream(CComPtr<Document> pDoc,

                                constchar* StorageName,

                                constchar* Stream2Delete)

{

    HRESULT hr ;

 

    CComPtr<IUnknown> pUnk;

    hr = pDoc->GetPrivateStorage(CComBSTR(StorageName),

                                VARIANT_FALSE,&pUnk);

 

   if(hr != S_OK)

  {

      //ERROR: unable to open Storage

      return hr;

   }

 

   CComQIPtr<IStorage> pStg(pUnk);

 

   //Perform deletion of the stream element

   hr = pStg->DestroyElement(CComBSTR(Stream2Delete));

 

   pStg->Commit(STGC_DEFAULT);

 

   return hr;

}

How can I Tell If a ComponentOccurrence is Excluded or Not in IAssembly

By Barbara Han

Issue

I'm trying to find out if a ComponentOccurrence is excluded or not in iAssembly, but did not find any property I could use. Is it possible?

Solution

You can use the iAssemblyTableRow.IsExcluded() function for this purpose. The code below assumes that the ActiveDocument is an iAssembly.

VBA code sample:

Sub testExclude()
Dim invAD As AssemblyDocument
Set invAD = ThisApplication.ActiveDocument
If invAD.ComponentDefinition.IsiAssemblyFactory Then
Dim invCO As ComponentOccurrence
For Each invCO In invAD.ComponentDefinition.Occurrences
Debug.Print invCO.Name & " is excluded = " & _
invAD.ComponentDefinition.iAssemblyFactory.DefaultRow.IsExcluded(invCO)
Next
End If
End Sub

VB.NET code sample:

Sub testExclude()

  Dim m_inventorApp As Inventor.Application = Nothing

  Dim m_quitInventor As Boolean = False

  ' 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)

    m_quitInventor = True

  End If

  Dim invAD As AssemblyDocument

  invAD = m_inventorApp.ActiveDocument

  If invAD.ComponentDefinition.IsiAssemblyFactory Then

    Dim invCO As ComponentOccurrence

    For Each invCO In invAD.ComponentDefinition.Occurrences

      System.Diagnostics.Debug.Write(invCO.Name & " is excluded = " & _      invAD.ComponentDefinition.iAssemblyFactory.DefaultRow.IsExcluded(invCO) & vbCr)

    Next

  End If

  If Not m_inventorApp Is Nothing AndAlso m_quitInventor = True Then

    m_inventorApp.Quit()

  End If

  m_inventorApp = Nothing

End Sub

 

Replace a ComponentOccurrence in a Sub Assembly

By Barbara Han

Issue

I have the following structure: "assembly->subassembly->part" and I'm trying to replace part with another part. The part occurrence is in Edit mode when I run the ComponentOccurrence.Replace() function, but instead of replacing the part, my code adds the new part to subassembly. What is wrong?

Solution

It's always worth having a look at the behaviour of the user interface.
In this particular case, when the SubPart is in Edit mode, then in the user interface the "Component->Replace" command is not available in the context menu of the Model Browser.
So, if you want to replace the subcomponent then edit its parent instead. Here is the sample code:

VBA code:

Sub replaceComponent()
Dim invAD As AssemblyDocument
Set invAD = ThisApplication.ActiveDocument
Dim invCO As ComponentOccurrence
Set invCO = invAD.ComponentDefinition.ActiveOccurrence
If Not invCO.ParentOccurrence Is Nothing Then invCO.ParentOccurrence.Edit
Call invCO.Replace("C:\Part1.ipt", True)
End Sub

Equivalent C# code:

public static void replaceComponent()

{

    try

    {

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

        AssemblyDocument invAD = app.ActiveDocument as AssemblyDocument;

        ComponentOccurrence invCO = invAD.ComponentDefinition.ActiveOccurrence;

        if (invCO.ParentOccurrence != null)

        {

            invCO.ParentOccurrence.Edit();

            invCO.Replace("c:\\Part1.ipt", true);

        }

    }

    catch

    {

    }

}

Set a new ObjectDefaultsStyle in a Drawing

By Wayne Brill

You may be having trouble setting a new ObjectDefaultsStyle in a Drawing. This could be because the ObjectDefaultsStyle can not be activated directly. It can via a DrawingStandardStyle however. Each DrawingStandardStyle has only one ObjectDefaultsStyle. When you activate a standard, you also set the active ObjectDefaultsStyle. These VBA and VB.NET examples create a new standard and a new ObjectDefaultsStyle for it. The Copy method needs to be used to create new standard and style.

VBA

Sub SetObjectDefaultsStyle()
    Const kStandardName = "My Standard"
    Const kObjDefaultsName = "My Defaults"
    Dim oDoc As DrawingDocument
   
    On Error Resume Next
   
    Set oDoc = ThisApplication.ActiveDocument
    Dim oStylesMgr As DrawingStylesManager
   
    Set oStylesMgr = oDoc.StylesManager
    Dim oStandard As DrawingStandardStyle
   
    Set oStandard = oStylesMgr.StandardStyles _
                             .Item(kStandardName)
   
    If oStandard Is Nothing Then
        Set oStandard = oStylesMgr.StandardStyles _
                       .Item(1).Copy(kStandardName)
    End If
   
    ' create object defaults
    Dim oObjDefaults As ObjectDefaultsStyle
    Set oObjDefaults = oStylesMgr. _
          ObjectDefaultsStyles.Item(kObjDefaultsName)
   
    If oObjDefaults Is Nothing Then
        Set oObjDefaults = oStylesMgr. _
         ObjectDefaultsStyles.Item(1). _
                  Copy(kObjDefaultsName)
    End If
   
    oStandard.ActiveObjectDefaults = oObjDefaults
   ' activate standard
    oStylesMgr.ActiveStandardStyle = oStandard

End Sub

VB.NET

Public Class Form1

 

    Dim m_inventorApp As Inventor.Application _

                                      = Nothing

 

    Private Sub Button1_Click(ByVal sender As  _

                                System.Object, _

                  ByVal e As System.EventArgs) _

                        Handles Button1.Click

 

        ' Get an active instance of Inventor

        Try

            m_inventorApp = System.Runtime. _

                   InteropServices.Marshal. _

       GetActiveObject("Inventor.Application")

 

        Catch 'Inventor not started

            System.Windows.Forms.MessageBox. _

             Show("Start an Inventor session")

            Exit Sub

        End Try

 

        'Call the Sub

        SetObjectDefaultsStyle()

    End Sub

 

    Public Sub SetObjectDefaultsStyle()

        Try

            Const kStandardName As String = _

                                  "MyStandard"

            Const kObjDefaultsName As String = _

                                   "My Defaults"

 

            Dim oDoc As DrawingDocument = _

                        m_inventorApp.ActiveDocument

            Dim oStylesMgr As DrawingStylesManager = _

                                    oDoc.StylesManager

            Dim oStandard As DrawingStandardStyle = _

                                               Nothing

            For Each style As DrawingStandardStyle _

                          In oStylesMgr.StandardStyles

                If String.Compare _

                  (style.Name, kStandardName) = 0 Then

                    oStandard = style

                    Exit For

                End If

            Next

            If oStandard Is Nothing Then

                oStandard = oStylesMgr. _

               StandardStyles(1)._Copy(kStandardName)

            End If

            Dim oObjDefaults As  _

                ObjectDefaultsStyle = Nothing

            For Each DefaultsStyle As  _

                                ObjectDefaultsStyle _

                   In oStylesMgr.ObjectDefaultsStyles

                If String.Compare _

              (DefaultsStyle.Name, kObjDefaultsName) _

                                              = 0 Then

                    oObjDefaults = DefaultsStyle

                    Exit For

                End If

            Next

 

            If oObjDefaults Is Nothing Then

                oObjDefaults = oStylesMgr. _

                    ObjectDefaultsStyles(1).Copy _

                                (kObjDefaultsName)

            End If

            oStandard.ActiveObjectDefaults = _

                                         oObjDefaults

            oStylesMgr.ActiveStandardStyle = _

                                            oStandard

        Catch

        End Try

    End Sub

End Class